SHELL63单元中文说明

Release 10.0 Documentation for ANSYS

SHELL63

Elastic Shell

弹性壳单元

SHELL63 Element Description

SHELL63单元描述

SHELL63 has both bending and membrane capabilities. Both in-plane and normal

loads are permitted. The element has six degrees of freedom at each node: translations

in the nodal x, y, and z directions and rotations about the nodal x, y, and z-axes. Stress

stiffening and large deflection capabilities are included. A consistent tangent stiffness

matrix option is available for use in large deflection (finite rotation) analyses. See

SHELL63 in the ANSYS, Inc. Theory Reference for more details about this element.

Similar elements are SHELL43 and SHELL181 (plastic capability), and SHELL93

(midside node capability). The ETCHG command converts SHELL57 and

SHELL157 elements to SHELL63.

SHELL63既具有弯曲能力又具有膜力，可以承受平面内荷载和法向荷载。本单元每个节点

具有6个自由度：沿节点坐标系X、Y、Z方向的平动和沿节点坐标系X、Y、Z轴的转动。

应力刚化和大变形能力已经考虑在其中。在大变形分析（有限转动）中可以采用不变的切向

刚度矩阵。其详细的特性请参考Section 14.63 of the ANSYS Theory Reference

。

近似的单元

有SHELL43，SHELL181(塑性能力)，SHELL93（包含中间节点）ETCHG命令可以将

SHELL57和SHELL157单元转换为SHELL63单元。

Figure 63.1 SHELL63 Geometry

Figure 63.1 shell63几何描述

x

IJ

= Element x-axis if ESYS is not supplied.

如果无ESYS则x

IJ

为单元X轴

x = Element x-axis if ESYS is supplied.

如果有ESYS则为单元X轴

SHELL63 Input Data

SHELL63输入数据

The geometry, node locations, and the coordinate system for this element are shown

in Figure 63.1: "SHELL63 Geometry". The element is defined by four nodes, four

thicknesses, an elastic foundation stiffness, and the orthotropic material properties.

Orthotropic material directions correspond to the element coordinate directions. The

element coordinate system orientation is as described in Coordinate Systems. The

element x-axis may be rotated by an angle THETA (in degrees).

单元SHELL63的几何形状、节点位置及坐标系如图63.1所示，单元定义需要四个节点、四

个厚度、一个弹性地基刚度和正交各向异性的材料。正交各向异性的材料参数的方向依据单

元坐标系，单元坐标系方向见Coordinate Systems章节。单元的X轴可以转动一个角度

THETA（度数）。

The thickness is assumed to vary smoothly over the area of the element, with the

thickness input at the four nodes. If the element has a constant thickness, only TK(I)

need be input. If the thickness is not constant, all four thicknesses must be input.

在单元的面内，其节点厚度为输入的四个厚度，单元的厚度假定为均匀变化。如果单元厚度

不变，只需输入TK(I)即可；如果厚度是变化的，则四个节点的厚度均需输入。

The elastic foundation stiffness (EFS) is defined as the pressure required to produce a

unit normal deflection of the foundation. The elastic foundation capability is bypassed

if EFS is less than, or equal to, zero.

弹性地基刚度(EFS)定义：在地基法线方向产生一个单位位移所需要的压力。如果EFS小于

或者等于0，则弹性地基的效应将被忽略。

For certain nonhomogeneous or sandwich shell applications, the following real

constants are provided: RMI is the ratio of the bending moment of inertia to be used

to that calculated from the input thicknesses. RMI defaults to 1.0. CTOP and CBOT

are the distances from the middle surface to the extreme fibers to be used for stress

evaluations. Both CTOP and CBOT are positive, assuming that the middle surface is

between the fibers used for stress evaluation. If not input, stresses are based on the

input thicknesses. ADMSUA is the added mass per unit area.

对于一些非均匀或者夹心壳的情况，本单元提供了以下实常数：RMI是由壳体本身的抗弯

刚度与按照输入厚度计算得出的抗弯刚度的比值，RMI默认为1.0。CTOP和 CBOT是从中

面到上下两面纤维的距离以用来计算应力。CTOP和 CBOT均为正数，假定中面位于用来

计算应力的上下两面纤维的中间，如果没有输入CTOP和 CBOT，应力根据输入的厚度进

行计算。ADMSUA为单位面积上的附加质量。

Element loads are described in Node and Element Loads. Pressures may be input as

surface loads on the element faces as shown by the circled numbers on Figure 63.1:

"SHELL63 Geometry". Positive pressures act into the element. Edge pressures are

input as force per unit length. The lateral pressure loading may be an equivalent

(lumped) element load applied at the nodes (KEYOPT(6) = 0) or distributed over the

face of the element (KEYOPT(6) = 2). The equivalent element load produces more

accurate stress results with flat elements representing a curved surface or elements

supported on an elastic foundation since certain fictitious bending stresses are

eliminated.

单元的荷载描述见Node and Element Loads（节点荷载和单元荷载）。压力可以作为表面荷

载，按照图SHELL63.1上显示的圆圈内数字表示的单元表面输入。压向单元的荷载为正荷

载。边界压力输入值为单位长度上的力。侧向荷载可能是一个作用在节点上的等效（集中）

单元荷载(KEYOPT(6) = 0)，或者是在分配在单元面上(KEYOPT(6) = 2)。在以平面单元代替

曲面的情况或者单元支撑在弹性地基上时，因为消去了一些假定的弯曲应力，等效单元荷载

可以得到更为精确的应力结果。

Temperatures may be input as element body loads at the "corner" locations (1-8)

shown in Figure 63.1: "SHELL63 Geometry". The first corner temperature T1

defaults to TUNIF. If all other temperatures are unspecified, they default to T1. If

only T1 and T2 are input, T1 is used for T1, T2, T3, and T4, while T2 (as input) is

used for T5, T6, T7, and T8. For any other input pattern, unspecified temperatures

default to TUNIF.

温度可以作为单元的体积力作用在图SHELL63.1上的（1～8）角点，第一个角点温度T1

默认为TUNIF，如果其他角点的温度没有指定，则默认为T1，如果只有指定T1和T2，T1

代表T1, T2, T3, T4； T2 代表T5, T6, T7, T8，如有其他输入格式，未指定的温度均默认为

TUNIF。

KEYOPT(1) is available for neglecting the membrane stiffness or the bending

stiffness, if desired. A reduced out-of-plane mass matrix is also used when the

bending stiffness is neglected.

如果需要的话，KEYOPT(1)可以用于忽略抗弯刚度或者忽略膜力刚度的情况。忽略弯曲刚

度时将运用减缩的出平面质量矩阵。

KEYOPT(2) is used to activate the consistent tangent stiffness matrix (that is, a

matrix composed of the main tangent stiffness matrix plus the consistent stress

stiffness matrix) in large deflection analyses [NLGEOM,ON]. You can often obtain

more rapid convergence in a geometrically nonlinear analysis, such as a nonlinear

buckling or postbuckling analysis, by activating this option. However, you should not

use this option if you are using the element to simulate a rigid link or a group of

coupled nodes. The resulting abrupt changes in stiffness within the structure make the

consistent tangent stiffness matrix unsuitable for such applications.

KEYOPT(2)用来在大变形分析中激活调和切线刚度矩阵（即：一个矩阵由主切线刚度矩阵

加上调和切线刚度矩阵而得）。在几何非线性分析如非线性屈曲或者后屈曲分析中，打开这

个选项可以更快得到收敛。不过，在模拟刚性杆或耦合节点时，不应该激活本单元的这个选

项，结构内刚度突然的变化使得调和切线刚度矩阵不适合这种情况。（KEYOPT(2)只能为0）

KEYOPT(3) allows you to include (KEYOPT(3) = 0 or 2) or suppress (KEYOPT(3)

= 1) extra displacement shapes. It also allows you to choose the type of in-plane

rotational stiffness used:

KEYOPT(3)允许你考虑(KEYOPT(3) = 0 or 2)或者抑制(KEYOPT(3) = 1)额外的位移形状。它

还允许你选择平面内转动刚度的类型：

•

•

•

KEYOPT(3) = 0 or 1 activates a spring-type in-plane rotational stiffness about

the element z-axis

KEYOPT(3) = 0 或1激活弹簧性质的单元 Z轴平面内转动刚度

KEYOPT(3) = 2 activates a more realistic in-plane rotational stiffness

(Allman rotational stiffness - the program uses default penalty parameter

values of d

1

= 1.0E-6 and d

2

= 1.0E-3).

KEYOPT(3) = 2 激活更实际的平面内转动刚度（Allman转动刚度――程序使用默认

的罚常数值为d1 = 1.0E-6 、 d2 = 1.0E-3）

•

Using the Allman stiffness will often enhance convergence behavior in large

deflection (finite rotation) analyses of planar shell structures (that is, flat shells or flat

regions of shells).

使用Allman刚度经常能加强在平面壳结构（即:平面壳或者壳里的平面部分）的大变形（有

限转动）分析中的收敛能力

KEYOPT(7) allows a reduced mass matrix formulation (rotational degrees of freedom

terms deleted). This option is useful for improved bending stresses in thin members

under mass loading.

KEYOPT(7)允许使用减缩质量矩阵（转动自由度被删除）。这个选项在质量荷载作用下的

薄壳中对改善弯曲应力很有用处。

KEYOPT(8) allows a reduced stress stiffness matrix (rotational degrees of freedom

deleted). This option can be useful for calculating improved mode shapes and a more

accurate load factor in linear buckling analyses of certain curved shell structures.

KEYOPT(8)允许使用减缩应力矩阵（转动自由度被删除）。这个选项在一些曲线壳结构的

线形屈曲分析中对改善模态形状合更精确的荷载倍数很有用处。

KEYOPT(11) = 2 is used to store midsurface results in the results file for single or

multi-layer shell elements. If you use SHELL,MID, you will see these calculated

values, rather than the average of the TOP and BOTTOM results. You should use this

option to access these correct midsurface results (membrane results) for those

analyses where averaging TOP and BOTTOM results is inappropriate; examples

include midsurface stresses and strains with nonlinear material behavior, and

midsurface results after mode combinations that involve squaring operations such as

in spectrum analyses.

KEYOPT(11) 是用来为单层或多层壳单元存储中面结果的结果文件。

如果你使用

SHELL,MID命令，你会看到这些计算值，而不是顶部和底部的平均结果。你可以使用这个

选项来访问这些正确的中面结果（膜结果）因为分析平均顶部和底部的结果是不恰当的。例

子包括中面材料非线性行为的应力应变以及涉及平方运算如频谱分析的模式组合后的中面

结果。

A summary of the element input is given in "SHELL63 Input Summary". A general

description of element input is given in Element Input.

单元输入摘要见下面的Input Summary（输入摘要），单元输入的一般性描述见Element Input

（单元输入）。

SHELL63 Input Summary

SHELL63输入摘要

Nodes 节点

I, J, K, L

Degrees of Freedom 自由度

UX, UY, UZ, ROTX, ROTY, ROTZ

Real Constants 实常数

TK(I), TK(J), TK(K), TK(L), EFS, THETA,

RMI, CTOP, CBOT, (Blank), (Blank), (Blank),

(Blank), (Blank), (Blank), (Blank), (Blank), (Blank),

ADMSUA

See Table 63.1: "SHELL63 Real Constants" for a description of the real

constants

Material Properties 材料属性

EX, EY, EZ, (PRXY, PRYZ, PRXZ or NUXY, NUYZ, NUXZ), ALPX,

ALPY, ALPZ (or CTEX, CTEY, CTEZ or THSX, THSY, THSZ), DENS,

GXY, DAMP

Surface Loads 面荷载

Pressures -- 压力

face 1 (I-J-K-L) (bottom, in +Z direction), face 2 (I-J-K-L) (top, in -Z

direction),

face 3 (J-I), face 4 (K-J), face 5 (L-K), face 6 (I-L)

Body Loads 体荷载

Temperatures -- 温度

T1, T2, T3, T4, T5, T6, T7, T8

Special Features 特殊特性

Stress stiffening应力刚化

Large deflection大变形

Birth and death单元生死

KEYOPT(1)

Element stiffness:单元刚度

0 --

Bending and membrane stiffness

弯曲刚度和膜力

1 --

Membrane stiffness only

仅考虑膜力刚度

2 --

Bending stiffness only

仅考虑弯曲刚度

KEYOPT(2) （只能为0）

Stress stiffening option:应力刚化选项

0 --

Use only the main tangent stiffness matrix when NLGEOM is ON. (Stress

stiffening effects used in linear buckling or other linear prestressed analyses

must be activated separately with PSTRES,ON.)

在NLGEOM 设为 ON时仅考虑主切线刚度矩阵（在线形屈曲或其他线形预应力分

析中考虑应力刚化效应必须另外激活PSTRES,ON.）（只能选0，见最后）

1 --

Use the consistent tangent stiffness matrix (that is, a matrix composed of the

main tangent stiffness matrix plus the consistent stress stiffness matrix) when

NLGEOM is ON and when KEYOPT(1) = 0. (SSTIF,ON will be ignored for

this element when KEYOPT(2) = 1 is activated.) Note that if

SOLCONTROL is ON and NLGEOM is ON, KEYOPT(2) is automatically

set to 1; that is, the consistent tangent will be used.

在（NLGEOM is ON 和 KEYOPT(1) = 0）时激活调和切线刚度矩阵（即：一个矩

阵由主切线刚度矩阵加上调和切线刚度矩阵而得）。当激活KEYOPT(2) = 1时

SSTIF,ON将被忽略。注意，当SOLCONTROL 设为 ON且 NLGEOM设为 ON

时KEYOPT(2)自动设为1，即自动激活调和切线刚度。

2 --

Use to turn off consistent tangent stiffness matrix (i.e., a matrix composed of

the main tangent stiffness matrix plus the consistent stress stiffness matrix)

when SOLCONTROL is ON. Sometimes it is necessary to turn off the

consistent tangent stiffness matrix if the element is used to simulate rigid

bodies by using a very large real constant number . KEYOPT(2) = 2 is the

same as KEYOPT(2) = 0, however, KEYOPT(2) = 0 is controlled by

SOLCONTROL, ON or OFF, while KEYOPT(2) = 2 is independent of

SOLCONTROL.

当SOLCONTROL 设为 ON，用于关闭调和刚度矩阵（即：一个矩阵由主切线刚

度矩阵加上调和切线刚度矩阵）。当单元用于模拟具有很大实常数的刚体时，关闭

调和刚度矩阵是有必要的。KEYOPT(2)=2同KEYOPT(2)=0，然而KEYOPT(2)=0

由SOLCONTROL设为ON或者OFF决定，而KEYOPT(2)=2和SOLCONTROL

命令之间是相互独立的。

KEYOPT(3)

Extra displacement shapes:特别位移形状

0 --

Include extra displacement shapes, and use spring-type in-plane rotational

stiffness about the element z-axis (the program automatically adds a small

stiffness to prevent numerical instability for non-warped elements if

KEYOPT(1) = 0).

考虑特别的位移形状，使用弹簧性质的单元Z轴平面内转动刚度（如果KEYOPT(1)

= 0，对非翘曲单元，程序自动加上一个小刚度以免数值不稳定）

Note

For models with large rotation about the in-plane direction,

KEYOPT(3) = 0 results in some transfer of moment directly to ground.

模型平面内有大旋转，

KEYOPT(3) = 0会导致一些弯矩传递直接接地。

1 --

Suppress extra displacement shapes, and use spring-type in-plane rotational

stiffness about the element z-axis (the program automatically adds a small

stiffness to prevent numerical instability for non-warped elements if

KEYOPT(1) = 0).

抑制特别的位移形状，使用弹簧性质的单元Z轴平面内转动刚度（如果KEYOPT(1) =

0，对非翘曲单元，程序自动加上一个小刚度以免数值不稳定）

2 --

Include extra displacement shapes, and use the Allman in-plane rotational

stiffness about the element z-axis). See the ANSYS, Inc. Theory Reference.

考虑特别的位移形状，使用单元Z轴Allman平面内转动刚度，详见14.43.6 of the

ANSYS Theory Reference

.

KEYOPT(5)

Extra stress output:特别应力输出

0 --

Basic element printout基本单元输出

2 --

Nodal stress printout节点应力输出

KEYOPT(6)

Pressure loading:压力荷载

0 --

Reduced pressure loading (must be used if KEYOPT(1) = 1)

减缩压力荷载（如果KEYOPT(1) = 1，则必须打开）

2 --

Consistent pressure loading

协调压力荷载

KEYOPT(7)

Mass matrix:质量矩阵

0 --

Consistent mass matrix

协调质量矩阵

1 --

Reduced mass matrix

减缩质量矩阵

KEYOPT(8)

Stress stiffness matrix:应力刚化矩阵

0 --

“Nearly” consistent stress stiffness matrix (default)

“近似”协调应力刚度矩阵（默认）

1 --

Reduced stress stiffness matrix

减缩应力刚度矩阵

KEYOPT(9) （只能为0，见最后）

Element coordinate system defined:定义单元坐标系

0 --

No user subroutine to define element coordinate system

无用户子程序定义单元坐标系

4 --

Element x-axis located by user subroutine USERAN

用USERAN定义单元坐标系

Note

See the Guide to ANSYS User Programmable Features for user written

subroutines

(用户子程序详见 ANSYS Guide to User Programmable Features)

KEYOPT(11)

Specify data storage:

指定数据存储:

0 --

Store data for TOP and BOTTOM surfaces only

仅存储顶面和底面的数据

2 --

Store data for TOP, BOTTOM, and MID surfaces

存储顶面、底面和中面的数据

Table 63.1 SHELL63 Real Constants实常数

No.

1

2

3

4

5

6

7

8

9

19

Name

TK(I)

TK(J)

TK(K)

TK(L)

EFS

THETA

RMI

CTOP

CBOT

Description

Shell thickness at node I

节点I壳厚度

Shell thickness at node J

节点J壳厚度

Shell thickness at node K

节点K壳厚度

Shell thickness at node L

节点L壳厚度

Elastic foundation stiffness

弹性基础刚度

Element X-axis rotation

单元X轴旋转角

Bending moment of inertia ratio

弯曲惯量比

Distance from mid surface to top

中面到顶面的距离

Distance from mid surface to bottom

中面到底面的距离

- - 10, ..., 18 (Blank)

ADMSUA

Added mass/unit area

附加质量/单位面积

SHELL63 Output Data

SHELL63输出数据

The solution output associated with the element is in two forms:

与单元有关的结果输出有两种形式：

Nodal displacements included in the overall nodal solution

•

包括在整个节点解中的节点自由度。

•

Additional element output as shown in Table 63.2: "SHELL63 Element

Output Definitions"

•

附加的单元输出，见单元输出定义。

•

Several items are illustrated in Figure 63.2: "SHELL63 Stress Output". Printout

includes the moments about the x face (MX), the moments about the y face (MY), and

the twisting moment (MXY). The moments are calculated per unit length in the

element coordinate system. The element stress directions are parallel to the element

coordinate system. A general description of solution output is given in Solution

Output. See the ANSYS Basic Analysis Guide for ways to view results.

在图中显示了几个应力输出项。输出包括X面(MX)的弯矩、Y面(MY)的弯矩、和扭矩（MXY）。

弯矩为单元坐标系内单位长度上计算所得。单元应力方向和单元坐标系统平行。对各种结果

输出的描述见结果输出Solution Output。描述结果的方法参见ANSYS Basic Analysis Guide

Figure 63.2 SHELL63 Stress Output

Figure 63.2 SHELL63 应力输出

x

IJ

= Element x-axis if ESYS is not supplied.

x = Element x-axis if ESYS is supplied.

The Element Output Definitions table uses the following notation:

单元输出定义表使用如下标记：

A colon (:) in the Name column indicates the item can be accessed by the Component

Name method [ETABLE, ESOL]. The O column indicates the availability of the

items in the file . The R column indicates the availability of the items in

the results file.

name 列表示该项目可以通过构成名字的方法来获得[ETABLE, ESOL]。第O 列表示该项有

效的说明在文件 中。R 列表示该项的结果显示在results 文件中。

In either the O or R columns, Y indicates that the item is always available, a number

refers to a table footnote that describes when the item is conditionally available, and a

- indicates that the item is not available.

无论在0 还是R 列中，Y 表示该项一直是可用的。数值表示描述哪里该项是选择性提供的

脚注，－表示该项不提供。

Table 63.2 SHELL63 Element Output Definitions单元输出定义

Name

EL

NODES

MAT

AREA

XC, YC, ZC

PRES

Definition

Element Number

单元号

Nodes - I, J, K, L

节点 - I, J, K, L

Material number

材料号

AREA

面积

Location where results are reported

结果输出点位置

O R

Y Y

Y Y

Y Y

Y Y

Y 1

Pressures P1 at nodes I, J, K, L; P2 at I, J, K, L; P3 at J, Y Y

I; P4 at K, J; P5 at L, K; P6 at I, L

P1

在节点 I, J, K, L; P2 在 I, J, K, L; P3 在 J, I; P4在K, J; P5

在 L, K; P6 在 I, L

TEMP

T(X, Y, XY)

M(X, Y, XY)

Temperatures T1, T2, T3, T4, T5, T6, T7, T8

温度 T1, T2, T3, T4, T5, T6, T7, T8

Y Y

Y Y

Y Y

Y -

Y Y

Y Y

Y Y

Y Y

Y Y

Y Y

In-plane element X, Y, and XY forces

平面内单元 X, Y, 和 XY 集中力

Element X, Y, and XY moments

单元X, Y, 和 XY 弯矩

Foundation pressure (if nonzero)

地基压力 (如果非0)

LOC

S:X, Y, Z, XY

S:1, 2, 3

S:INT

S:EQV

EPEL:X, Y, Z,

XY

Top, middle, or bottom

上表面, 中面, or 下表面

Combined membrane and bending stresses

合成的弯曲和模的应力

Principal stress

主应力

Stress intensity

应力强度

Equivalent stress

等效应力

Average elastic strain

平均弹性应变

Name

EPEL:EQV

EPTH:X, Y, Z,

XY

EPTH:EQV

Definition

Equivalent elastic strain [2]

等效弹性应变

Average thermal strain

平均热应变

Equivalent thermal strain [2]

等效热应变

O R

- Y

Y Y

- Y

1. Available only at centroid as a *GET item.

只有在质心作为*GET项时可用

2.

The equivalent strains use an effective Poisson's ratio: for elastic and thermal

this value is set by the user (MP,PRXY).

等效应变应设定柏松比：对于弹性和热

柏松比用MP，PRXY命令输入。

Table 63.3 SHELL63 Miscellaneous Element Output混合单元输出项

Description

Nodal Stress Solution

Names of Items Output

TEMP, S(X, Y, Z, XY), SINT, SEQV

O R

1-

1. Output at each node, if KEYOPT(5) = 2, repeats each location

如果KEYOPT（5）＝2，则输出每个节点的值

Table 63.4: "SHELL63 Item and Sequence Numbers" lists output available through

the ETABLE command using the Sequence Number method. See The General

Postprocessor (POST1) in the ANSYS Basic Analysis Guide and The Item and

Sequence Number Table in this manual for more information. The following notation

is used in Table 63.4: "SHELL63 Item and Sequence Numbers":

“SHELL63项目和序号表”中列出了在后处理中可通过ETABLE命令加参数及数字序

号的方法定义可列表察看的有关变量的细则。详细参见《ANSYS基本分析指南》中有关“The

General Postprocessor (POST1)”和“The Item and Sequence Number Table”部分。下面是表

格的一些使用说明：

Name

output quantity as defined in the Table 63.2: "SHELL63 Element Output

Definitions"

指在“SHELL63单元输出数据说明表”中的有关变量。

Item

predetermined Item label for ETABLE command

命令ETABLE中使用的参数。

E

sequence number for single-valued or constant element data

对于单值或常数型单元数据的序列号；

I,J,K,L

sequence number for data at nodes I,J,K,L

节点I,J,K,L处数据的序列号。

Table 63.4 SHELL63 Item and Sequence Numbers输出项和序列号

Output Quantity Name

TX

TY

TXY

MX

MY

MXY

P1

P2

P3

P4

P5

P6

Top

S:1

S:2

S:3

S:INT

S:EQV

Bot

S:1

S:2

S:3

S:INT

S:EQV

NMISC

NMISC

NMISC

NMISC

NMISC

- 21

- 22

- 23

- 24

- 25

26

27

28

29

30

31

32

33

34

35

36

37

38

39

40

NMISC

NMISC

NMISC

NMISC

NMISC

- 1

- 2

- 3

- 4

- 5

6

7

8

9

10

11

12

13

14

15

16

17

18

19

20

ETABLE and ESOL Command Input

Item

SMISC

SMISC

SMISC

SMISC

SMISC

SMISC

SMISC

SMISC

SMISC

SMISC

SMISC

SMISC

E

1

2

3

4

5

6

- 9

- 13

- 18

-

-

-

-

I

-

-

-

-

-

-

J

-

-

-

-

-

-

10

14

17

20

-

-

K

-

-

-

-

-

-

11

15

-

19

22

-

L

-

-

-

-

-

-

12

16

-

-

21

24 - 23

SHELL63 Assumptions and Restrictions

SHELL63单元假设及使用限制

•

•

•

•

•

•

•

Zero area elements are not allowed. This occurs most often whenever the

elements are not numbered properly.

单元不能面积为0。这种情况经常出现在单元被非正常计数时。

Zero thickness elements or elements tapering down to a zero thickness at any

corner are not allowed.

0厚度单元或者在任何角点逐渐变细到0厚度也不被允许。

The applied transverse thermal gradient is assumed to vary linearly through

the thickness and vary bilinearly over the shell surface.

施加的横向热梯度假定为沿厚度方向线形变化，在壳体表面则双线形变化。

An assemblage of flat shell elements can produce a good approximation of a

curved shell surface provided that each flat element does not extend over more

than a 15° arc. If an elastic foundation stiffness is input, one-fourth of the total

is applied at each node. Shear deflection is not included in this thin-shell

element.

一系列相互之间角度小于15°的平面壳单元可以很好的模拟一个曲线壳。如果输入一

个弹性地基刚度，则每个节点作用1/4，剪切变形在这种薄壳里不被考虑。

•

•

A triangular element may be formed by defining duplicate K and L node

numbers as described in Triangle, Prism and Tetrahedral Elements. The extra

shapes are automatically deleted for triangular elements so that the membrane

stiffness reduces to a constant strain formulation. For large deflection analyses,

if KEYOPT(1) = 1 (membrane stiffness only), the element must be triangular.

一个三角形单元，如Triangle, Prism and Tetrahedral Elements里描述，用重合K、L

节点的方法形成。对于三角形单元，额外的形状自动被删除，膜力刚度缩减为常应

变公式。对于大变形分析，如果KEYOPT(1) = 1（仅考虑膜力刚度），单元必须是

三角形。

•

•

For KEYOPT(1) = 0 or 2, the four nodes defining the element should lie as

close as possible to a flat plane (for maximum accuracy), but a moderate

amount of warping is permitted. For KEYOPT(1) = 1, the warping limit is

very restrictive. In either case, an excessively warped element may produce a

warning or error message. In the case of warping errors, triangular elements

should be used (see Triangle, Prism and Tetrahedral Elements). Shell element

warping tests are described in detail in tables of Applicability of Warping

Tests and Warping Factor Limits in the ANSYS, Inc. Theory Reference.

KEYOPT(1) = 0 or 2时四节点单元必须在准确的平面上。不过，一小点的出平面公

差可能使单元具有轻微的翘曲形状。KEYOPT(1) = 1适度的翘曲单元将在输出中产

生一个警告信息。如果翘曲非常严重，将产生一个致命的信息结果，应该考虑使用

三角形单元。详见Triangle, Prism and Tetrahedral Elements。如果集中质量矩阵公式

被指定

•

If the lumped mass matrix formulation is specified [LUMPM,ON], the effect

of the implied offsets on the mass matrix is ignored for warped SHELL63

elements.

•

（[LUMPM,ON]），对于翘曲SHELL63单元，质量矩阵的implied offsets将被忽略。

•

SHELL63 Product Restrictions

SHELL63产品限制

When used in the product(s) listed below, the stated product-specific restrictions

apply to this element in addition to the general assumptions and restrictions given in

the previous section.

如果在下面列出的ANSYS产品中使用这种单元时，除了上面列出的一般假设和约束外，对

这种单元还有其它规定的产品特殊限制。

ANSYS Professional.

•

•

•

•

•

•

•

•

The DAMP material property is not allowed.

DAMP材料属性不允许

The only special features allowed are stress stiffening and large deflection.

唯一允许的特殊特性是应力刚化和大变形

KEYOPT(2) can only be set to 0 (default).

KEYOPT(2) 只能设为0（默认的）

KEYOPT(9) can only be set to 0 (default).

KEYOPT(9) 只能设为0（默认的）